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Inventor - Component View Item Numbers – Methods and Suggestions

33 REPLIES 33
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Message 1 of 34
Scotty87
8247 Views, 33 Replies

Inventor - Component View Item Numbers – Methods and Suggestions

Hi all,

After a bit of thought I’ve decided to do a write up on issues with item numbers in Inventor drawings. My reasons for this are that I want to know if there any ways to do what I want to do that I haven’t discovered, describe some current methods that some of you might find useful, and get support and/or criticism for a new feature that I am going to present.

 

As a draftsman with 4 years + experience with Inventor, I have come to know the program fairly well and regard it highly.

 

There is however one major flaw with the drawing environment: The inability (there are workarounds, which I will get to shortly) to attach an item number to component detail views that reference the BOM of their parent assembly.

This may seem trivial, but is a subject that keeps coming up, not just from Inventor users but also from other design office personnel, allocation staff and manufacturing workers.

 

I won’t rule out the possibility that this feature exists (if it does, please enlighten me!), but I would like to know why such an important feature has been omitted. Legal/copyright reasons? Marketing reasons? It’s not possible to program it that way? Not seen as important? In development?

 

Whatever the case, I will now discuss 3 workaround methods, followed by my own suggestion as to how I believe this feature could/should be included.

 

Method 1: iProperties Item Reference

Using this method, the item column and item bubbles reference an iProperty (such as Part Number or Stock Number) rather than the Item Number found in the BOM. A base view of an assembly is placed on a drawing, followed by base views of its parts. A parts list referencing the assembly is then created, and item balloons are attached to all parts on the assembly view and all component base views.

Advantages of this method include:

  • Ability to attach item balloons to each component base view.
  • Ability to include the item number in component view labels.

Disadvantages include:

  • Item numbers must be entered manually.
  • Item number is an iProperty; if a component is being used in multiple drawings, it retains its original item number. If the item number is changed to suit a new drawing’s BOM, the original drawing’s BOM will also update.
  • Does not allow for automatic renumbering in the parts list editor.

Method 2: Component View Representations

In the assembly, a new view representation is created for each component, in which visibility for every other component is switched off. A base view of the assembly is placed on a drawing with the relevant view representation selected for each part detail.

Advantages:

  • Allows ballooning of component views using BOM Item Number.
  • Quantity can be added to balloons and view labels.

Disadvantages:

  • Creation of view representations is time consuming.
  • A new view representation must be created for each new component.
  • Visibility of newly placed components must be manually deselected.
  • iProperties in view label reference parent assembly
  • Inability to detail flat pattern views.

Method 3: Weldment Detail

This method is similar to the view representation method, however the views are created automatically. It has the disadvantage that a weldment must be created for it to be of any use; as such it has no use for fastened assemblies that require component details.

 

These 3 methods all have their pros and cons, and really only appear to be workarounds for the problem at hand.

 

Now to my suggestion:

 

COMPONENT VIEWS

 

First, a standard base view of an assembly is placed on the drawing.

In the drawing environment, on the views panel of the drawing tab, there will be a button titled “Component Views”.

Pressing this button will bring up a prompt that says “select source view”.

The user then clicks on the base view on the assembly, and a dialogue box appears.

The box has a list of the assembly’s components, each next to a check box. The user then checks the required components, or checks “select all”.

The user then places each component view 1 by 1, selecting orientation as they go.

Item balloons can now be added to the component views; the number reflects the item number in the parts list of the parent view.

BOM data can also be added to the view label via “BOM Properties” in the drop down menu, and “Component Properties” references the iProperties of the component; Model Properties still allows the parent assembly to be referenced.

The component view can be turned into a standard base view by right clicking it and selecting “convert to base view”. I would also endorse the possibility of converting base views to component views.

 

I’m no expert on the programming side of things, but I don’t see why this isn’t possible; all the information is there, it seems like it’s a matter of getting it all in the one place.

 

Please let me know what you think about the component views idea. Preferably quote one of the following points

  • Great idea! Autodesk, take note.
  • Sounds good, but needs more thought.
  • Not that important, but it can’t hurt to have it.
  • Some good points, but lots of flaws; I am happy without it.
  • No good, completely unnecessary / totally flawed.

 

Thanks for reading, constructive criticism is greatly appreciated.

33 REPLIES 33
Message 2 of 34
PaulMunford
in reply to: Scotty87

I think that the answer may be semantic - but this is how I am coming to understand it.

 

The assembly Item No. is only meant to be used to call out the part numbers on the current drawing (or set of drawings). i.e. the drawings for one assemblyThis is how engineering drawings have always worked.

 

If you are creating a 'piece part' drawing, then you shouldn't need to refer to an assembly item No., because only one part is shown on the drawing.

 

To reference the part to the assembly drawing you would use a unique Part Number.

 

So the drill down would look like this.

 

Assembly drawing > Parts list > Item No. > Part Number

 

In theory, you don't need to go the other way, beacuse a part could be used in many different assemblies. Each assembly however, is unique.

 

I'm not saying that there is no need for the feature as you describe, I'm only saying that Inventor was designed to work using a traditional engineering process.

 


Autodesk Industry Marketing Manager UK D&M
Opinions are my own and may not reflect those of my company.
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Message 3 of 34
jtylerbc
in reply to: PaulMunford

Paul's explanation is correct.  Inventor's way of handling the item numbers is optimized for a manufacturing environment with unique parts identified by part numbers.

 

In that sort of an environment, each of these parts gets its own individual drawing, rather than being a "detail view" related to an assembly drawing.  The assembly item number is not shown on this drawing, because it isn't needed and in many (if not most) cases there will actually be more than one.

 

What we're really talking about here is a difference in drawing styles between manufacturing and fabrication.  Inventor's setup is optimized for the manufacturing conventions, and requires a bit of improvisation for fabrication.  Having come from a manufacturing-based company to a fabrication based one a couple of years ago, these differences in thinking are something I deal with regularly.

 

Since we had some inconsistency in our drawing formats anyway, I picked one of the used conventions that was more Inventor-friendly and made it the standard.  We don't use the Item Number at all on our fabrication drawings.  Instead, we use "Mark Number", which is really just a renamed "Part Number" column in the parts list.  I then put the Part Number iProperty in the view labels for the details.

 

Isn't really a true solution for what you're asking for, but it sidesteps the issue and works for us.

Message 4 of 34

Hi Scotty87,

 

A few quick questions:

 

  • What version of Inventor are you using?
  • Are you open to using ilogic to help with this?
  • Can you provide a simple example data set and/or screen shots that will illustrate your goal(s)?

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

Message 5 of 34
PaulMunford
in reply to: jtylerbc

Thanks for that jtylerbc, I'm glad I wasn't baring up the wrong tree!

 

That's and interesting point that you make about manufacturing Vs Fabrication. I also work infabrication and I have trying to get the Assembly Item No. to do somrthing I am begining to think it wasn't inteded for. 

 

It's good to get some validation 🙂

 

Paul

 


Autodesk Industry Marketing Manager UK D&M
Opinions are my own and may not reflect those of my company.
Linkedin Twitter Instagram Facebook Pinterest

Message 6 of 34
jtylerbc
in reply to: PaulMunford

Taking my explanation just a bit further:

 

We annotate these types of drawings with a balloon style that uses the Part Number property rather than the Item Number.  So, there is never actually an "Item Number" anywhere on the drawing.

 

I actually have parts lists and balloon styles set up for both types of formats.  We do steel fabrication (frames) as well as final assembly of other components (hydraulics, etc) for our equipment.  The method I've been describing works well for the steel fabrication drawings, and looks like one of the more common formats of our previous AutoCAD work.

 

However, it is very messy for purchased parts, which might have long model codes as the part number.  The normal way of using Item Numbers and balloons in Inventor works much better for these drawings.  I use two different Standards to set the default styles appropriately for the particular drawing.

 

It's a very simple fix if you can get away with using the Part Number field instead of the Item Number.  Even if you don't want to put it in the view label, and instead want to use a balloon on the detail views, the Part Number property is still the same whether you're looking at the part in an assembly or by itself.

Message 7 of 34
Scotty87
in reply to: jtylerbc

Thanks for the replies!

 

@ Paul Munford and jtylerbc:

 

FYI, I'm from Australia (guessing you guys are from the US?), so my drafting techniques are going to be based on Aus standards; for the most part I'm not sure how other countries operate.

In any case, I've done drafting work for 4 companies in 4 different industries (marine oil, recycling, water purification and currently coal mining), and every one of them will create a drawing that contains an assembly or weldment and on the following sheets (sometimes, as in my attachments, the same sheet) or a new drawing file, detail views of the constituent parts. Some parts do get a drawing all to themselves though, as do subassemblies.

As for fabrication drawing vs. manufacturing drawings, even if Inventor is optimised for one over the other, there is no reason why it shouldn't be able to better accommodate the other. Both have their merits and are important for manufacturing.

The concept of using unique iProperties as mark numbers would definitely be good in some applications, but it's not really what I'm getting at. The company I'm with now uses part numbers that are usually the same as the file number to identify parts (see attachments), however the long part numbers are difficult to read and usually don't follow any logical order. Also, I mentioned in my original post using iProperties to identify parts; the difference being that your suggestion implies unique mark numbers whereas I was implying a substitute for item numbers.

Also note that the component views feature that I suggested shouldn't in any way affect the way you create drawings/views etc; it would still allow you to create a drawing exactly as you do today, but with the added option of creating linked views that can be annotated with data from both the part itself and its parent's BOM.

 

@ Curtis_Waguespack:

 

I'm currently using Inventor 2012 Professional (full version at work, student version at home).

Yeah, I'm open to using iLogic. I've managed to get component quantities using it, but no such luck with item numbers.

See attached files.

Fig1 shows what I want to achieve, using both part iProperties and BOM properties (Item, Qty).

Fig2 shows a drawing similar to what I would create where I work now.

BTW, I'm currently reading Mastering Inventor 2012 and it's great! Only up to chapter 4 and I'm already picking up on lots of little things that I had previously overlooked. 

Message 8 of 34
jtylerbc
in reply to: Scotty87

I wasn't saying it shouldn't do both, was just explaining the reasoning behind what it currently does.  It would be nice to have the option of both for those who need it.  With the amount of structural steel stuff in the Content Center, it would seem to make sense to make the drawing annotation a bit more fabrication-friendly.

 

I think iLogic is probably going to be your best bet.  Another possibility, which I've seen used on some of our older Inventor drawings, is to use View Representations.  Instead of placing views of the individual parts, you would create View Reps in the assembly that turn off all but one part, then place a view of that.  Since your view is still the assembly, the item numbers still work correctly.  I think this is the closest currently-existing option to your "component view" suggestion.

 

However, if you have any information you want to pull from the part into the view label (part number, etc), this method will mess that up (because the view technically isn't of the part).

Message 9 of 34
Scotty87
in reply to: jtylerbc

Re: first paragraph, I (almost) agree completely. Only rather than thinking it would be a nice addition, I'm thinking "why the f*** haven't they done this already?!"

 

Case in point: One of the pre production/allocation staff members where I currently work has gone to the extent of adding item balloons to each part base view in red pen on printed drawings so he has an easy way of linking the views to the parts list. Also as I've already mentioned, this isn't an isolated need; 4 out of 4 places I've worked at include multiple part details on a single drawing.

 

Re: second paragraph, I have played around with iLogic and have managed to get quantities out of it but still can't do anything with item numbers. So far I only have limited experience with iLogic though, and wouldn't be surprised if it could solve my issues. As for view representations, I mentioned this method in my original post, including the reasons why I think it is insufficient. I do agree however that it probably is the closest existing method to what I want to achieve.

Message 10 of 34

Hi Scotty87,

 

Thanks for the screen shots, that helps a great deal.

 

Let's take this one step at a time. To start off here is an iLogic rule that will create a view rep that islolates each part in the assembly. If more than one instance of the part is present it isolates just the first one. If a Default view rep is present the rule honors the visibility settings you might have adjusted previously. If no Default view rep is found then it creates one and sets all parts visible.

 

Likewise if a view rep that has the same name as one of the parts is present then the rule honors it and makes no adjustments, but will create a view rep for each part name that isn't present as a view rep. Once the view reps are created they are locked

 

Give it a test and see what you think. I currently have the display updating as the view reps are created so you get some visual feedback, but let me know if that runs too slowly.

 

I'll look at the drawing views next (as time permits).

 

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com


 

 

 

'define current document
Dim openDoc As Document
openDoc = ThisDoc.Document

' set a reference to the assembly component definintion.
' this assumes an assembly document is open.
Dim oAsmCompDef As AssemblyComponentDefinition
oAsmCompDef = ThisApplication.ActiveDocument.ComponentDefinition

'look at all of the components in the assembly
Dim oCompDef As Inventor.ComponentDefinition = openDoc.ComponentDefinition

'define the first level components collection
Dim oCompOcc As Inventor.ComponentOccurrence 

'define view rep 
Dim oViewRep As DesignViewRepresentation

'define an arraylist to hold the list of  view rep names
Dim NameList As New ArrayList()

'Look at the view reps in the assembly
For Each oViewRep in oAsmCompDef.RepresentationsManager.DesignViewRepresentations
'set the list of names to the array list
NameList.add(oViewRep.Name)
Next

'check for a Default view rep and create it if not found
If Not NameList.Contains("Default") Then
	'create Default view rep 
	oViewRep = oAsmCompDef.RepresentationsManager.DesignViewRepresentations.Add("Default") 
	oViewRep.ShowAll
	oViewRep.Activate
End If

'zoom all
ThisApplication.CommandManager.ControlDefinitions.Item("AppIsometricViewCmd").Execute

'look at all of the unique parts in the assembly
For Each docFile In openDoc.AllReferencedDocuments
	If docFile.DocumentType = 12290 Then '12290 is the part document enumurator
	'locate the last backslash position in the full file name
	Dim FNamePos As Long
	FNamePos = InStrRev(docFile.FullFileName, "\", -1) 
	'remove path from part file name 	
	Dim docFName As String
	docFName = Right(docFile.FullFileName, Len(docFile.FullFileName) - FNamePos)         
	'remove extension from part file name 
	ShortName = Left(docFName,  Len(docFName) - 4)   
		'check to see if the arraylist contains the desired view rep
		If Not NameList.Contains(ShortName) Then
		'create new View Rep 
		oViewRep = oAsmCompDef.RepresentationsManager.DesignViewRepresentations.Add(ShortName)
		oViewRep.Activate
		oViewRep.Locked = False	
		Else if NameList.Contains(ShortName) Then
		'reference existing View Rep 
		oViewRep = oAsmCompDef.RepresentationsManager.DesignViewRepresentations.Item(ShortName) 
		oViewRep.Activate
		oViewRep.Locked = False
		End If
		'look at all of the occurences
		For each oCompOcc in oCompDef.Occurrences
		'locate the colon position in the occurence name
		oCompOccPos = InStrRev(oCompOcc.Name, ":") 
		'set occurence name to everything left of the colon
		oOccName = Left(oCompOcc.Name, oCompOccPos -1) 
			'set visible if name matches first occurence
	      		If oCompOcc.Name = ShortName & ":1"  Then
			oCompOcc.Visible = True
			ThisApplication.ActiveView.Update()
			Else
			oCompOcc.Visible = False
			ThisApplication.ActiveView.Update()
			End If
		Next
	End If
	'lock view rep
	oViewRep.Locked = True	
Next

'set Default View Rep active
oAsmCompDef.RepresentationsManager.DesignViewRepresentations.Item("Default").activate

 

Message 11 of 34
dan_inv09
in reply to: Scotty87

If there was an add-in or something that would quickly create a view rep for each part

If you could make added parts not affect certain view reps after creation

If the grayed out boxes in the text dialog worked (maybe a little smarter, but let's start with just "work")

 

Unless I'm reading your solution wrong, those are the differences between it and method 2

 

We shouldn't go asking for brand new features when all we need is small enhancements (fixes) to an existing one.

[It seems like they went, "Time's up, people. Put your pencils down!" every time they wanted a new feature in the upcoming release. Plus if they start on something new who knows what might get messed up.]

 

 

 

(For your last point for method 2, I've always had to create a new ("separate") base view for a flat pattern. Am I missing something?)

Message 12 of 34

Thanks for the code Curtis.

I've just created a rule in an assembly file and typed the code in (tried to copy paste but got about 6 errors), and when I try to run it I get the error "Object reference not set to an instance of an object".

I'm still a bit of a noob with iLogic/VBA, but I'm picking it up.

Message 13 of 34

Hi Scotty87,

 

Here's the rule in a text file. Hopefully the errors were just due to the copy/paste from the forum. If you still see errors after copying and pasting from the text file and running the run in a simple assembly just let me know.

 

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

 

Edit: I just noticed a flaw in this rule that I'll need to fix at some point (if you two instances of a part in the assembly (PartA:1 and PartA:2) and you delete instance one (PartA:1), the rule does not make a view rep. I'll need to fix it so that it looks for the first instance of each part, rather than instance " :1" of each part.

Message 14 of 34

Hey Curtis,

Sorry to be a pain but is that post supposed to contain an attachment?

Cheers.

Message 15 of 34

Hi Scotty87,

 

Ooops! Sorry about that. Smiley Embarassed

 

Here it is.

 

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com


Message 16 of 34
Scotty87
in reply to: dan_inv09

Thanks for that! It's working well so far.

Message 17 of 34
rkeller
in reply to: Scotty87

YES! YES! 

We need to be able to have the item numbers be carried through to other views.  It gives much more continuity to the drawing set.  

It would be great if we could access the item number you would find within the bill of materials in our own symbols allowing us to give much needed information to the fabricators without confusing them.

Message 18 of 34

Sorry for digging up a very old thread (plus I just realized I had participated in it).

I don't know if I ever used the code before but I just tried it and if we can sort out one thing I will definitely use it a lot.

 

I am working with a housing assembly which has top and bottom subassemblies (and some other junk). It created view reps for each part but all views show nothing except the one part that happens to be in the top level.

Is there an edit which I can do so it will show the parts when they are in subassemblies?

 

Because of that I have to unlock each view to fix them. I could just delete the lock line from the code to fix that, so that's not to bad, or if I could multi-select to unlock that would be great (that's nothing to do with the code).

And the browser appears to be linked to the view rep, so every time I activate another view it collapses everything. Could something in the code be affecting it, or if I had them expanded before I ran it would that fix this annoyance?

 

This is really awesome, I was really dreading this but now it's a whole lot quicker - if it could also drop everything into a drawing too (that would probably have to be a separate code - can anyone tell me what are the best current resources for learning to write my own?) - then we just need it dimension itself and they can lay me off, ha ha.

Message 19 of 34

This is the insanity of INVENTOR! While it tries to cater to the ENGINEERING side of things, it seems to ignore some of the "real world" users that use it to create manufacturing drawings.

 

I've used INVENTOR for over 10 years, at several companies and I think we get a lot of good production from the software. However, we do not do "piece part", single item drawings that link back to a "part number" drawing in order to keep everything neat and in an ENGINEERING standard drawing set.

 

We start off with some standard sized steel member (content center parts: angle, tubes, beams) and have our own library of sheet goods (fiberglass, abs, pvc) as well as a library of custom extruded parts (angles, tubes). This all works awesome inside INVENTOR's modeling world.

 

However, the bulk of these parts are almost NEVER used in two different assemblies! Everything we do is custom. And it seems to be the way shops run where I've worked. THIS IS NOT A UNIQUE SITUATION!

 

Every Parts lists/BOM has items 1,2,3...... But these parts are unique to this project, and this assembly. To NOT have the ability to export the item number to a symbol is INSANE! Currently we have the filename of the part exported to a symbol that we use for quality control checking. But our "part number" portion is manually entered, and SHOULD be automatic! And this symbol SHOULD include the "part number" and "quantity"!!!

 

Additionally the item quantity is not exportable! We have a person manually go through drawings and add quantities beside the part number balloon manually (with a pen). So the shop personnel can quickly total the parts needed and NOT reference the BOM/PARTS LIST every time. This is increasingly important depending on the size of the assembly!

 

To have the ability to export the part number and the quantity to a symbol should be TOP PRIORITY with the INVENTOR programmers. It's something that has been missing from the software since the begninning!

Message 20 of 34
280122
in reply to: Curtis_Waguespack

Hi Curtis,

i am using your I-logic rule to create automatic view rep in my assemblyies and sub assemblies. but i am always getting this errors below.

 

Any idea of how i can solve them ?

 

Thanks for your time;D

 

 

Alessandro

 

Error message

 

Error in rule: Automatic view creation rule, in document: BG_Komplett.iam

unknown error (Exception from HRESULT: 0x80004005 (E_FAIL))

 

More Info

 

System.Runtime.InteropServices.COMException (0x80004005): unknown error (Exception from HRESULT: 0x80004005 (E_FAIL))
   at System.RuntimeType.ForwardCallToInvokeMember(String memberName, BindingFlags flags, Object target, Int32[] aWrapperTypes, MessageData& msgData)
   at Inventor.DesignViewRepresentation.set_Locked(Boolean )
   at LmiRuleScript.Main()
   at Autodesk.iLogic.Exec.AppDomExec.ExecRuleInAssembly(Assembly assem)
   at iLogic.RuleEvalContainer.ExecRuleEval(String execRule)

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